Can you force sketch dimension to be angular?

[pimm]

Every once in a while I run into a situation where I need to add an angular dimension to a sketch and it wants to change it to linear.

The problem appears to be that the angle is less than a degree.

Here is the sketch prior to adding the dimension.  There isn't a lot of difference of height but there is a difference.

Here is what happens after the dimension.  You can see that the shading hasn't updated on the right corner.

How do you force an angular dimension?

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[pushkarkhanna]

Hi Paul,

The workaround to adding angular dimensions for very small angle is to create an angular dimension from some other reference (maybe a normal plane or ref) which gives a bigger dimension. Then we can just select the dimension & use replace command to change the reference to desired one.

Pushkar

[StephenW]

The way I do it is to create the sketch with a much larger exaggerated angle, add the angle dimension and then change the angle dimension to the desired small number.

[rzukowski · Accepted solution]

Try the config.pro option:

minimum_angle_dimension

I have mine set to 0.1

Rick Z.

[pimm]

Actually everyone's answer here is correct.

I like your answer Rick because it doesn't require the slight work around.

I tried searching for a config.pro option on this by searching by angular instead of angle prior to asking this question.  In the past I've left the sketch partially unconstrained, but sometimes that doesn't work out well.

Finally this works the way it should!  Thanks.

[Pieface]

I have a 0.2 degree angle and after changing the config.pro to "minimum_angle_dimension 0.1" I still cannot get the dim to place properly.  I have tried everything I can think of including zooming way out and in.  Prior to Creo you could zoom in real closely and it might flip the dim to angular.  I tried a dummy line and edit attachment as well as selecting a datum that was far enough away that Creo might see it as an angle.  Edit attachment after using a dummy line just sent the dim back to linear.

[StephenW]

Did you try the exaggerated angle first to get the placement as you desire and then change the dimension to 0.2. Creo (and if you go all the way back to pro/e before the intent manager) have never liked slight angles. It want's the world to be straight and square!!!

[Pieface]

Did not realize the main topic was sketcher.  The geometry is complete and I am creating the dimension in the drawing.  Thank you for replying.

[RonSt.Pierre]

It sounds like you already have this feature in the model

Instead of "creating" a dimension, try "showing" the dimension.

Showing pulls the model definition directly.

[Pieface]

We had a solid model and I was asked if I could do it in sheet metal to get a flat pattern.  Sure, where is dwg?  I have not modeled in sheet metal for many years and am happy to learn what I have missed.

The back wall is not straight.  608.8 on top and 614.6 on bottom.

This means when I attach the side walls they are at an angle of 0.186 degrees.  So, when I add the top flange if I wanted it to be parallel to the Top Datum I needed to compensate on the angle.

After modeling I was advised by the flat they meant without the side bends.  These bends would be done internally and the remainder of the part would be purchased outside.  I told them I would have to remodel for the driving dim's to display on the purchased part dwg.  They said it is an old part and no one cares.  Well, us CAD folks do!  So, I obliged and created a bend back on both of the side walls resulting in this:

It displays like this on the print:

Note 7 uses an analysis feature to state the angle is .26 degrees.  Since the feature was created in another view, it is not displayable.  2+/-1 is sufficient.  I do wish I could create the dim, but it does not appear to be possible unless I have not found the trick.  I do not know if the create angular dim issue is sheet metal or Creo?

[SteveFowler]

Thanks All, I have been using the work around for years. This is great!